CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   icem cfd tetra meshing error (http://www.cfd-online.com/Forums/ansys-meshing/90881-icem-cfd-tetra-meshing-error.html)

joegi.geo July 22, 2011 21:43

icem cfd tetra meshing error
 
hi,

I am tryiing to mesh a quite complex geometry uisng tetra meshing (delaunay), but in the status window I get this message:

Initialization failed

Then the meshing crash/fail. I wonder what does it means this initialization failed message and how can i avoid this error. I am starting the volume mesh from a surface.

Regards,

Joel

PSYMN July 23, 2011 13:48

Delaunay requires an initialization before the volume filling can begin.

During this phase, it checks for single edges (holes), overlapping elements and other problems.

You should do these checks before hand and make sure your mesh is a water tight volume. Once you sort out your surface mesh problems, the volume mesh will generate.

Best regards,

Simon

joegi.geo July 23, 2011 14:48

Hi Simon,


Thanks a lot for your reply. So at this point what should I do with these erros? I have uncovered faces, missing internal faces, penetrating elements, multiple edges, single edges and overlapping elements. Should I fix then automatically, erase them, groud them????????????


joel

PSYMN July 24, 2011 00:17

Create subsets for each one... I only use autofix for the last one (disconnected nodes or what ever it is called).

Then right click on each subset in the tree and add layers... This is just to give you an idea of what is actually going on there...

For instance, single edges just means shell elements that have an edge not connected to anything... The auto fix just deletes the elements, which is fine if they are just a junk tab (like a hanging chad from 2000), but if they are the edge of a hole or baffle, you don't want those deleted, you will just have a growing single edge problem. Instead create the subset and then add a few layers so you can diagnose properly... If it is the edge of a baffle (intentional and not a problem), you can just remove that clump of cells from the subset and look for other problems... If it is a hole in the surface, you can consider repairing the geometry and meshing again, or perhaps it would be easier to mesh edit your way out (Edit mesh => repair => Mesh from edges)...

And so on... Problem by problem.

If you have too many problems, you may want to go and think about your initial geometry. If you brought in in from an IGES file, consider other CAD formats... Pretty much anything is better than IGES. ACIS comes in very clean and could save you a ton of work.

If the geometry is hopeless, then perhaps a patch dependent method is not the best to start with. Try switching you shell meshing method to something that can tolerate the slop you are feeding it. You will find that Patch independent surface mesh works well with the sizing function and is a good starting point for delaunay volume mesh...

joegi.geo July 25, 2011 10:24

Hi simon,

Thanks a lot for the tips, I am continuously learning new stuff in icemcfd. I wonder if you can take a look at the geo and give me some ideas of what could be the problem. Pretty much I think the geometry is watertight but when I try to use local refinement the meshing is always failing. I get a mesh when I use coarse parameters.

Regards,

joel

joegi.geo July 26, 2011 08:34

Hi Simon,

I wonder what is the meaning of this message. SHould I worry about it?


rounding points to prescribed points
cannot round any tvertex to prescribed point PART_2_EDGE.709

PSYMN July 29, 2011 11:00

The message just means it couldn't place a vertex on that point... It can happen if you have too many points in an area and the mesh is not fine enough to resolve all of them.

From a side conversation, I heard that your leakage problems were because you had not placed material points in the solids... That shouldn't cause this problem (it should automatically assume those are ORFN), but I am glad you are able to move on.


All times are GMT -4. The time now is 05:21.